Only calculate your drift/error [assuming it is repeatable] and make the holes that much smaller in software so that they come out the size you want.[Verify tool diameter with calipers as well, that itself could solve or at least explain your problem]

Speaking from a machining standpoint a down cut bit would be the worst possible bit to drill a hole there is no where for the swarf to leave the hole. What is the material? I am assuming wood. Even a properly sized drill bit will drill and over sized hole. When precision holes are needed usually the hole is drilled under sized and reamed to the proper diameter speaking for harder materials than wood. A bored hole can be made to be pretty accurate and with experimentation would probably be made to accommodate your arbor size. Generally a .005"-.010" over sized hole will make a good slip fit. Interference fits are usually .002"-.005" undersized. 4MM is a fairly small hole depending on thickness of the material you may be able to find a small bit to bore the hole I would recommend a spiral ramp into the hole using an up cut bit.

My machine is not perfect, so when milling holes, I always start with a hole that is 0.1mm smaller and when finished, still on the machine table, I try how it fits with the thing that is going into the hole. But I always make Gcode's for the next sizes, 0.5mm, 0.1mm, 0.15mm, 0.2mm bigger. It takes just one minute to offset a circle a few times and make couple of Gcodes and run them if necessary.

On most machines, if you lift up on the router, you will see that the bit tip moves parallel to the gantry travel direction. This same thing happens when the bit is pushed into the material to make a hole, the result being that the entry hole ends up elongated. The answer, of course, is to use a smaller bit and enlarge the hole as described in the other answers.

Good judgement comes from experience.Experience comes from bad judgement.

FixitMike wrote:On most machines, if you lift up on the router, you will see that the bit tip moves parallel to the gantry travel direction. This same thing happens when the bit is pushed into the material to make a hole, the result being that the entry hole ends up elongated. The answer, of course, is to use a smaller bit and enlarge the hole as described in the other answers.

Sorry Mike, I don't follow. Why does the bit move in X or Y when shifting Z?

Paul RowntreeWarpDriver, StandingWave, Topo and gadgets available at PaulRowntree.weebly.com

PaulRowntree wrote:Sorry Mike, I don't follow. Why does the bit move in X or Y when shifting Z?

It moves in Y when you apply a force in the Z direction. The motor carriage hangs off the side of the cross beam. When you pull up on the motor, the resulting torque on the beam (Plus any deflection in the carriage) causes it to twist in the YZ plane and the the bit tip to move in the Y direction. Plunging into the material causes the same upward force on the carriage.

The amount of movement may be trivial, or it can be quite obvious on machines like the Shark. One's choice of bit can affect the amount of movement, a downcut bit would probably increase the problem.

Just to be sure I knew what I was talking about, I ran a quick test. I cut two holes in hard maple, using a 1/4" diameter upcut spiral bit, .625 deep with the Drilling Toolpath. The results were elongated circles. They measured .251" in the X direction and .259" in the Y direction. Note that my Shark Pro Plus has has Paul's bearing rail modification using the Glacern Machine Tools supported linear ball bearing rails, which makes it considerably stiffer than the stock machine.

Good judgement comes from experience.Experience comes from bad judgement.